Aerospace News Abbott Aerospace SEZC Ltd

Composite Modeling and Analysis Part 4. – Joints

A version of this article first appeared in the February 2020 edition of our free newsletter, to subscribe click here

We return to composite (and other structure) finite element modelling
and tackle joints in this issue. To state the obvious joints are where
different pieces of structure are joined to each other.

For most joint modelling we are interested in extracting the loads from
the model at the joint interface and carrying out an external calculation to
give a margin of safety.

This is because the behaviour of joint is more complex than the general
structure and a finite element model requires a high degree of complexity to
represent all of the aspects and features of a joint (bonded or mechanically
fastened). It is much more efficient to make the stiffness of the area of the
joint broadly representative and design the mesh to make it easy to extract the
local loads.

At least that’s the correct approach for larger scale models. For
smaller scale models I have seen ( and created) detailed models of mechanical
fasteners and adhesive bond lines. But whatever those more detailed models tell
me I always end up relying on extracting the loads and running a hand check to
make sure the joint will be good.

Adhesively bonded joints:

For adhesively bonded joints in large scale models we will model the
flange that is bonded into the skin mesh. This is done to better model the
stiffness of the vonded joint interface. This also helps with the local
stiffness of this region for the buckling solution

We have found that if the core ends in the correct position and the
bonded flange against the skin is not modelled you can start to get compression
buckles of the stretch of uncored skin. This is because the bonded flange
creates additional out of plane bending stiffness that stops the compression
buckle in these regions.

The element loads form the rib (or frame) web can ex extracted and used
to check the bondline for shear transfer and peel in the following way.

This is the simplest and most robust way we have found to deal with
adhesive bonds at a large scale.

For detailed models we will sometimes model the adhesive as solid
elements, this is the finite element model for the edge of transparency:

One of these interfaces uses a bonded joint, in this case we modelled
the joint as a set of solid elements that share the nodes of the laminate elements
either side of the joint. This does not help us determine if the bond is likely
to fail, but it is a more accurate representation of the stiffness of the
intact bondline.

The von mises stress in the solid elements representing the bondline
looks like this:

This indicates there is a peak von mises stress of around 5,000psi. In
general we use 1,000psi as the average bond shear ultimate allowable.

And we generally assume 200lb/in ultimate bond peel allowable.

Interpreting whether the bond line would fail is not simple given the
above results. How do these results translate to our 1,000psi average shear
stress allowable? This test article carried 1.5 times the load applied to the
finite element model without failing this bondline.

We also went in to pass the ultimate pressure load for the fuselage with
this design of windshield installation.

So we ignored the results from the elements that modelled the adhesive,
but it gave the local region the correct stiffness for the resolution of
results we required from the laminate.

Mechanical Joints

In general differentiate between rivets and bolts. We treat rivets like
bondlines – we model them as a continuous connection at the nodes and extract
the load flows from the local elements and calculate the peak load on the
rivets.

For bolts at major structural interfaces we generally mode the bolts as
CBUSH elements.

We center a node in the fastener hole of the fitting using a REB2
elements.

We create a mating node at the position of the hole in the mating item.

We connect the two nodes with a CBUSH Spring/Damper Element.

A typical fitting to wing spar is shown below:

We use a fictional set of stiffnesses for the CBUSH element:

We do not leave any of the stiffnesses as zero. This is a trick to avoid
unrestrained degrees of freedom. Of course you check the deflection of the
model and if the deflection is excessive this may be down to a spring element
degree of freedom allowing the model to run but also allowing very large
deflections……

So we force the theoretical bolt to transfer tension, shear and bending
(but not torsion) as if it were infinitely stiff.

We do not take account of the local theoretical fastener spring
stiffness. This is because the stiffness is partly provided by the local
stiffness of the interfacing items, in this case the wing fitting and the rear
spar web. If we account for these in the fastener stiffness there is some
element of double accounting.

This approach is easier and likely just as inaccurate.

As we do not model material plasticity it this scale of the model we are
not taking account of load redistribution at the point of bearing yield so the
linear model is not representative so the level of accuracy is further degraded
for ultimate level loads.

For all of the joints we have sized using this approach we have seen no
failures on test of the fasteners at the interface or the interface components
at the fastener locations.

We do have to think about the moments carried by the elements
representing the fasteners though. There is a method for doing this, this is
defined in section 12.2.8 of our structures textbook:

In this method you can override the ‘M’ value with the resulting moment
from the CBUSH element results and set the ‘P’ as the tension load. ‘B’ should
be the distance from the center of the hole to the edge of fitting. This will
give you the effective total tension carried by the fastener.

We use this method of modelling fasteners for all resolution of models.
I have been involved in projects where the fasteners are modelled using higher
order methods (non linear gap elements, solid models with contact surfaces) but
I am not convinced that they add a greater degree of accuracy when all the
variables of a real life fastener installation and joint behaviour is
considered.

What is your experience with the FE modelling of joints? We would love
to hear from you.

Your email address will not be published. Required fields are marked *

Comment

Name *

Email *

Website

Composite Modeling and Analysis Part 4. – Joints

A version of this article first appeared in the February 2020 edition of our free newsletter, to subscribe click here

We return to composite (and other structure) finite element modelling
and tackle joints in this issue. To state the obvious joints are where
different pieces of structure are joined to each other.

For most joint modelling we are interested in extracting the loads from
the model at the joint interface and carrying out an external calculation to
give a margin of safety.

This is because the behaviour of joint is more complex than the general
structure and a finite element model requires a high degree of complexity to
represent all of the aspects and features of a joint (bonded or mechanically
fastened). It is much more efficient to make the stiffness of the area of the
joint broadly representative and design the mesh to make it easy to extract the
local loads.

At least that’s the correct approach for larger scale models. For
smaller scale models I have seen ( and created) detailed models of mechanical
fasteners and adhesive bond lines. But whatever those more detailed models tell
me I always end up relying on extracting the loads and running a hand check to
make sure the joint will be good.

Adhesively bonded joints:

For adhesively bonded joints in large scale models we will model the
flange that is bonded into the skin mesh. This is done to better model the
stiffness of the vonded joint interface. This also helps with the local
stiffness of this region for the buckling solution

We have found that if the core ends in the correct position and the
bonded flange against the skin is not modelled you can start to get compression
buckles of the stretch of uncored skin. This is because the bonded flange
creates additional out of plane bending stiffness that stops the compression
buckle in these regions.

The element loads form the rib (or frame) web can ex extracted and used
to check the bondline for shear transfer and peel in the following way.

This is the simplest and most robust way we have found to deal with
adhesive bonds at a large scale.

For detailed models we will sometimes model the adhesive as solid
elements, this is the finite element model for the edge of transparency:

One of these interfaces uses a bonded joint, in this case we modelled
the joint as a set of solid elements that share the nodes of the laminate elements
either side of the joint. This does not help us determine if the bond is likely
to fail, but it is a more accurate representation of the stiffness of the
intact bondline.

The von mises stress in the solid elements representing the bondline
looks like this:

This indicates there is a peak von mises stress of around 5,000psi. In
general we use 1,000psi as the average bond shear ultimate allowable.

And we generally assume 200lb/in ultimate bond peel allowable.

Interpreting whether the bond line would fail is not simple given the
above results. How do these results translate to our 1,000psi average shear
stress allowable? This test article carried 1.5 times the load applied to the
finite element model without failing this bondline.

We also went in to pass the ultimate pressure load for the fuselage with
this design of windshield installation.

So we ignored the results from the elements that modelled the adhesive,
but it gave the local region the correct stiffness for the resolution of
results we required from the laminate.

Mechanical Joints

In general differentiate between rivets and bolts. We treat rivets like
bondlines – we model them as a continuous connection at the nodes and extract
the load flows from the local elements and calculate the peak load on the
rivets.

For bolts at major structural interfaces we generally mode the bolts as
CBUSH elements.

We center a node in the fastener hole of the fitting using a REB2
elements.

We create a mating node at the position of the hole in the mating item.

We connect the two nodes with a CBUSH Spring/Damper Element.

A typical fitting to wing spar is shown below:

We use a fictional set of stiffnesses for the CBUSH element:

We do not leave any of the stiffnesses as zero. This is a trick to avoid
unrestrained degrees of freedom. Of course you check the deflection of the
model and if the deflection is excessive this may be down to a spring element
degree of freedom allowing the model to run but also allowing very large
deflections……

So we force the theoretical bolt to transfer tension, shear and bending
(but not torsion) as if it were infinitely stiff.

We do not take account of the local theoretical fastener spring
stiffness. This is because the stiffness is partly provided by the local
stiffness of the interfacing items, in this case the wing fitting and the rear
spar web. If we account for these in the fastener stiffness there is some
element of double accounting.

This approach is easier and likely just as inaccurate.

As we do not model material plasticity it this scale of the model we are
not taking account of load redistribution at the point of bearing yield so the
linear model is not representative so the level of accuracy is further degraded
for ultimate level loads.

For all of the joints we have sized using this approach we have seen no
failures on test of the fasteners at the interface or the interface components
at the fastener locations.

We do have to think about the moments carried by the elements
representing the fasteners though. There is a method for doing this, this is
defined in section 12.2.8 of our structures textbook:

In this method you can override the ‘M’ value with the resulting moment
from the CBUSH element results and set the ‘P’ as the tension load. ‘B’ should
be the distance from the center of the hole to the edge of fitting. This will
give you the effective total tension carried by the fastener.

We use this method of modelling fasteners for all resolution of models.
I have been involved in projects where the fasteners are modelled using higher
order methods (non linear gap elements, solid models with contact surfaces) but
I am not convinced that they add a greater degree of accuracy when all the
variables of a real life fastener installation and joint behaviour is
considered.

What is your experience with the FE modelling of joints? We would love
to hear from you.

Subscribe To Our Monthly Newsletter

Enter your email address to stay informed on our company activities, useful industry news, updates to the Technical Library, new spreadsheets, and more...

* indicates required

Email Address *

First Name

Last Name

Please Help us To Maintain, Expand and Improve The Technical Library

The Abbott Aerospace Technical Library is made possible by generous donations from our users. Please help us to maintain, improve and expand the library by making a contribution, giving us the means to expand our free technical library to include even more useful tools and references.

To make a one-time donation, select the PayPal button below. A donation of any amount is greatly appreciated.

Technical Library FAQs

Who are you?
We are the engineers from Abbott Aerospace.

Why do You do this for free?
A lot of the library material does not originate with us so, with good conscience, we cannot charge for that part of the library. There are issues with commercializing the material that we create, copy protection, customer support and pricing at the right level. By making everything available free of charge it lets us concentrate on content.

How is the library funded?
The library is funded using revenue from the engineering service side of Abbott Aerospace and by the donations of the people who find the library useful.

What should I do if I think I see a copyright violation in any of the library materials?
Please contact us immediately and give us specific information about your concern

What should I do if I think I find an error in any of the library materials?
Please let us know immediately

I would like to help the library by volunteering my time. How do I do that?
At the present time we are unable to accept any offers of help. In the future we would like to work with a group of volunteer engineers. At this time we have not developed the digital infrastructure to make this possible. You can help by making a donation of any size.

I would like to help by donating materials I have collected or created. How do I do that?
Let us know what you have and if it meets our criteria we will gladly accept it and give you a name credit if you choose.

What is the acceptance criteria for the library?
For any material to be added to the library it must me the following criteria

It must not already be in the library

Where the material is not authored by the contributor it must be the demonstrated to be in the public domain or where the material is created by the contributor it must reference an available public domain source.

It must be either a Adobe PDF document, a Microsoft Excel spreadsheet or a Microsoft Excel add-in file. Other types of files can be considered.